This tutorial was completed using ANSYS 7.0
The purpose of the tutorial is to show the how to use substructuring in ANSYS.
Substructuring is a procedure that condenses a group of finite elements into one super-element.
This reduces the required computation time and also allows the solution of very large problems.

A simple example will be demonstrated to explain the steps required, however, please note that this model is not one which requires the use of substructuring.
The example involves a block of wood (E =10 GPa v =0.29) connected to a block of silicone (E = 2.5 MPa, v = 0.41) which is rigidly attached to the ground.
A force will be applied to the structure as shown in the following figure.
For this example, substructuring will be used for the wood block.

The use of substructuring in ANSYS is a three stage process:

Generation PassGenerate the super-element by condensing several elements together.
Select the degrees of freedom to save (master DOFs) and to discard (slave DOFs).
Apply loads to the super-element

Use PassCreate the full model including the super-element created in the generation pass.
Apply remaining loads to the model.
The solution will consist of the reduced solution tor the super-element and the complete solution for the non-superelements.

Expansion PassExpand the reduced solution to obtain the solution at all DOFs for the super-element.

Note that a this method is a bottom-up substructuring (each super-element is created separately and then assembled in the Use Pass).
Top-down substructuring is also possible in ANSYS (the entire model is built, then super-element are created by selecting the appropriate elements).
This method is suitable for smaller models and has the advantage that the results for multiple super-elements can be assembled in postprocessing.

Since both the super-element and the non-superelement were created independently, they contain similarly numbered nodes (ie both objects will have node #1 etc.).
If we bring in the super-element with similar node numbers, the nodes will overwrite existing nodes from the non-superelements.
Therefore, we need to offset the super-element nodes

Determine the number of nodes in the existing model

Select Utility Menu > Parameters > Get Scalar Data ...

The following window will appear. Select Model Data, For Selected set as shown.

Fill in the following window as shown to set MaxNode = the highest node number

Note that only the deformation for the super-elements is plotted (and that the contour intervals have been modified to begin at 0).
This results agree with what was found without using substructuring (see figure below).

The above example was solved using a mixture of the Graphical User Interface (or GUI)
and the command language interface of ANSYS. This problem has also been solved using the
ANSYS command language interface that you may want to browse. Open the .HTML version, copy
and paste the code into Notepad or a similar text editor and save it to your computer. Now go to
'File > Read input from...' and select the file. A .PDF version is also available for
printing.